Surface transition steps. Why?

[wildcat99]

Hello everyone:

 

We just cut our first pattern today. It all went well except for the finish cut. Some surfaces have a definite step, ~.080", at the transition to another surface. These are not just "blend lines" which I was told to expect.

 

The problem areas just happen to be where I split surfaces in MasterCam using projected curves. There are nice, smooth transitions at the split lines that came in with the original model, however. Some of you may remember I had trouble splitting surfaces, but managed to get it done.

 

I was using Scallop Finish cuts with a 1/4" ball nose, Tip Comp was set to Tip for all. The part was basically a half cylinder boss with the top surface split longways into thirds. The center surface was cut 3-ax from the top plane. The two side surfaces were cut 3-ax from planes in the isometric views. The transition at these surfaces is one of the problem areas.

 

Has anyone seen this before? At this point, we don't know which surfaces are correct (did we cut too much or not enough?). Thanks in advance for your suggestions, we may be able to correct this before we unbolt it from the machine.

 

(Using 8.1.1 Mill Level 3. Everything looked fine in Backplot and Verify.)

 

[ 06-06-2002, 01:27 AM: Message edited by: wildcat99 ]

[Guest CNC Apps Guy 1]

Wildcat,

 

I'm guessing that the mis-match is coming from the machine. Try doing a Flow 5 Ax on the surfaces(all at once and I'd be willing to bet the problem will go away.

[wildcat99]

I don't believe a Flow 5ax will work on all the surfaces at once for clearance reasons. This was my original approach with no luck. Cadcam showed me how to cut each section separately with Flow5ax.

 

But, I ended up cutting the part 3ax on rotated tool planes because I knew how to make this work and was certain there would be no crashes.

 

The two outside sections were cut in mirrored "isometric" planes. The center was cut in the top plane. There should be a smooth, continuous transition between these. The problem is the right section is cut deeper than the center which is cut deeper than the left section.

 

So it's stair-stepped for some reason. It's almost like our y-axis shifted .080" between cuts.

 

Any other ideas? Does what I've described bring back bad memories for anyone else?

[chico]

Could it be an encoder problem or a table location feedback issue? These are both machine issues that could be hard to duplicate.

 

Just wanted to throw that out there. Good Luck.

 

Chico

[wildcat99]

Thanks for the input so far. We still don't know why we have mis-matched surfaces, but we are going to try and salvage the important part of this pattern.

 

James, Cadcam, anyone...

 

WC_PATTERN CADCAM.MC8 is on the FTP in MC8 files.

Is it possible to cut the blue surfaces with Flow5ax all at once? The tool needs to be tilted so the head doesn't hit the "base" board. I've tried several combinations of lead/lag and side tilt angles with no luck. Can this be done or am I barking up the wrong tree? Thanks for your help.

[cadcam]

Wildcat I was going to ask you for the file. thanks will look right now.

[Scott Bond]

Wildcat I was going to ask you for the file. thanks will look tonight.

[cadcam]

Ok I know what happened to you.

You wrote one program moved about the other to planes.

I just found out that your part is not TYP on both side when I split the surface and tried some thing.

You will need to split the surface for what you wanted and program them by them self’s or use boundrys.to Sep the area by programs.

YOU must use the surfaces that are there do not Mirror or rotate planes this is what happens on this part.

 

Ps still playing with the file for 5axis but need to go teach class will go over it in the morning sorry.

 

[ 06-06-2002, 06:02 PM: Message edited by: cadcam ]

[wildcat99]

Huh???

 

Are you saying the part is not symmetrical? It is not centered on the "base" board, but we don't cut the base board. The part itself (everything protruding out of the baseboard) should be symmetrical, though.

 

I don't understand what you are saying about rotating tool planes. I used the surfaces that were there, no mirrored toolpaths or anything like that...

[cadcam]

quote:

---

The two outside sections were cut in mirrored "isometric" planes.

---

Hey what’s this sir?

This were I got some of my thoughts as I was playing with your file.

 

May I have a copy of the file you used to make the cuts that had the trouble?

 

Will give you more tomorrow. just got home from teaching time for BED

 

[ 06-07-2002, 12:58 AM: Message edited by: cadcam ]

[wildcat99]

I don't know if I have all the terminology quite right. But what I did was create a circle in space in the iso view and used this to define one tool plane. I then selected surfaces on the part to cut from this plane.

 

I mirrored that circle in space about the part center and used the new circle to define the 2nd tool plane. I then selected surfaces on the other side of the part to cut from this plane.

 

Is this a bad way to cut a part? Does tool orientation matter that much when cutting surfaces? If I select surfaces that have smooth transitions and tell it to cut with the tip of the tool, shouldn't it cut those same surfaces no matter what angle the tool is at?

 

Anyway, I will put WCPATTERN_2.ZIP on the FTP. This has the original toolpaths. In the meantime we are checking the machine and our C-axis looks suspicious. I'm hoping it is off and we can recut using just the finish paths from the same posted file after adjusting the machine. But you have me wondering if it still may be a CAM problem. Thanks for your help. Bear with me, I'm still a newbie at all this.

[wildcat99]

Never mind....

 

You called it James:

quote:

---

I'm guessing that the mis-match is coming from the machine.

---

Today we found our C-axis was off which would cause the stair-stepping in the part. We hadn't noticed this till now, but we hadn't cut a pattern till now, let alone a symmetrical one.

 

Thank you to all who helped me on this. I'm confident my Mastercam toolpaths and posted file are OK. The truth will be revealed Monday when we re-cut.....the bondo is drying as we speak.